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Patterning a stubborn cut....


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I have a part that I'm working on that will not cooperate. This is probably something really basic but I'm having a hard time seeing what the problem is.

The main protrusion is a disk like shape. It has a cut in it that is more or less like a radial 'pie' section except that it does not cut all the way to the center axis, or all the way to the outer surface. The sides of the 'pie' are not exactly in the radial direction so I can't do an angular dimension to them to use for the pattern direction. What I've done is to draw a centerline that is constrained to the axis of rotation of the protrusion (or more accurately to the two normal datums in the sketch) and dimensioned the cut off of it. This centerline has an angular dimension to one of the normal datums.

Patterning the cut should be no problem. I think I should be able to pick the angular dimension and blamo, but no dice. Sometimes it will do 2 cuts, sometimes 4, but never the 15 that I want.

Help me see outside this tiny box I'm in!!!
Don't use a sketch dimension for your pattern leader. Instead, when you're creating your top/bottom reference for the sketcher, make a datum on the fly ProE2001) or create a datum during your selection (Wildfire). Use this dimension for patterning. When pattering, always start with the highest mode (general, varying, identical) and change type (e.g. until the pattern fails. The highest type (general allowa pattern features to intersect, reference different surfaces etc. THe higher the type the bigger the file size of your part/assy will be. Pro/E doesn't see circles, it only sees 2 curves that go together to make up a circle, so once the pattern gets past 180
I always use general pattern, the difference in file size and regen time are not worth the extra headaches recovering from failed regens.

I agree with pjw about always using a make datum for your sketch plane and/or reference plane for radial patterns. It's not a bad idea for all patterns.
I got it to work, but I'm not sure how. I tried doing what you said several different ways before I was able to make it work. It seems to matter a lot as to when you define the datum. I think I ended up creating the datum plane on the fly just before sketching the first cut. This creates an auto group of the cut and the datum. Then I patterned the auto group, not just the cut. Does this sound right? Thanks for your help!
Sounds like you are using WF (auto-group). When using WF, yes you have to pattern the auto group using a group pattern in order for it work. This is because all the references must be patterned as a group, including the datum plane that defines the sketch orientation. Pre-WF you could use the embedded datum-on-the-fly when creating the feature and create a simple feature pattern. Much easier! And lower feature count also!
>>datum-on-the-fly when creating the feature and create a simple feature pattern. Much easier! And lower feature count also!

Anyone think that PTC will capitulate and bring back DOTF ???

I admit the DOTF concept took a little bit of adjusting to but boy was it useful for patterning, for assembling, for compound cuts & holes etc, etc..

Classic case of throwing the baby out with the bath water..
>>...when creating the feature and create a simple feature pattern...

I gotta admit that the new 'direction' and 'axis' patterns in WF2 are sweet. You don't need any kind of datum at all (on-the-fly or otherwise).
I gotta admit that the new 'direction' and 'axis' patterns in WF2 are sweet.

Yeah, but DOTF could be used for much more.

Does ref pattern work okay ???
The reference pattern functionality works the same in WF 1.0 and 2.0 as it did in 2001.

The new direction and axis patterns are sweet and simple, eliminates the whole need to make datums when creating or redefining features. My only apprehension regarding direction patterns is that less discriminating users are going to create unwanted parent-child relationships when creating a direction pattern... and we all know the downside of choosing bad references.